CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   ANSYS Meshing & Geometry (http://www.cfd-online.com/Forums/ansys-meshing/)
-   -   [ICEM] faces are missorinted.. repair holes (http://www.cfd-online.com/Forums/ansys-meshing/119833-faces-missorinted-repair-holes.html)

m5edr June 25, 2013 21:58

faces are missorinted.. repair holes
 
3 Attachment(s)
Dear experts,
I have a small problem , it took long time for solving and i couldn't solve it :(


When I run the mesh ( Tetra, unstructured and Robust (octree) meshing techniques) a massage appeared in monitored screen "faces are missorinted" and then ICEM show me "repair holes" massage box "image1"

Notes:
1-There is no holes in my geometry (it a single blade inside a big 120o enclosure sector) and i am also run "repair geometry" before
2-The zone where the problem originates is >> a common edges between two couple of surface "image2"
3- I searched in cfd-online search for " faces are missorinted" but I found only one thread and it was useless for me :(
Finally, I attached the Icem file
Thanks in advance

m5edr June 27, 2013 00:24

Any help pls.

kad June 27, 2013 07:51

- set proper mesh sizes on all surfaces or parts, especially in the hub region
- delete all points and curves permanently
- run "Build Diagnostic Topology" with the default value it gives you
- set curve sizes (this is not a must)
- then run octree again

Edit:
When defining intersecting thin cuts, remember to have the curve between the two parts in another part.

diamondx June 27, 2013 11:12

The holes is right here:

https://dl.dropboxusercontent.com/u/35161486/hole.JPG

can you fix it ??? just delete that green surface and create surface from curve...
Let me know if you can't

diamondx June 27, 2013 11:14

wait sorry that was not a hole. i did check the full geometry. let me investigate more

sadjad.s June 27, 2013 11:26

Answer
 
4 Attachment(s)
As Ali said it seems that that surface was a problem, but by inactive/active that surface, the problem is gone!
One of the edges is not associated well.
I chose build up topology of 0.001 and it was corrected.
I then run Octree mesh.
There was no problem. I use Ansys v14.5.

kad June 27, 2013 11:42

1 Attachment(s)
I think there is no actual hole in the geometry. The problem may occur from topology and inproper mesh sizes. Try my suggested method, it works. I have attached the corrected files. Now, just set more mesh sizes to capture every detail of your geometry.

diamondx June 27, 2013 12:10

in my case the problem came from the thin cut, i added inter1 to pressure-side and inter2 to suction-side and the problem is gone.

m5edr July 9, 2013 06:52

Quote:

Originally Posted by kad (Post 436333)
- set proper mesh sizes on all surfaces or parts, especially in the hub region
- delete all points and curves permanently
- run "Build Diagnostic Topology" with the default value it gives you
- set curve sizes (this is not a must)
- then run octree again.

Thanks Kad for replay,

I tried this method But it didn't work also
Then i tried the 2nd method you stated it (below)

Quote:

Originally Posted by kad (Post 436379)
I think there is no actual hole in the geometry. The problem may occur from topology and inproper mesh sizes. Try my suggested method, it works. I have attached the corrected files. Now, just set more mesh sizes to capture every detail of your geometry.

where all curves and point collected in Geom part. It work until specific mesh size the error appear again (o.k i accept this mesh size and no problem)

thanks again

m5edr July 9, 2013 06:56

Quote:

Originally Posted by diamondx (Post 436385)
in my case the problem came from the thin cut, i added inter1 to pressure-side and inter2 to suction-side and the problem is gone.

thanks diamondx for replay But i need to seperate sides parts from inter parts for the sake of FLEUNT Data presentaion ( i need to represnt pressure variation on pressure-side and suction-side alone)

i tried many times to separate them in fluent but i failed (On the contrary, merge is an easy process in fluent)

thanks again

kad July 9, 2013 09:45

2 Attachment(s)
Wait, I think i found a hole in the geometry. There is a short gap between pressure and suction side of the blade. Octree does not mind the gap as long as elements are big enough.

m5edr July 9, 2013 10:05

Quote:

Originally Posted by kad (Post 438691)
Wait, I think i found a hole in the geometry. There is a short gap between pressure and suction side of the blade. Octree does not mind the gap as long as elements are big enough.

how can i fix it?

kad July 9, 2013 10:23

1 Attachment(s)
In ICEM it is very hard to fix. First you could go back to your CAD tool and try to fix it. Or try another exchange format.

You can also reverse the normal process. You can extract geometry from an existing mesh. I gave it a short try and it worked. Not all areas are good. So you could develope a mesh with your old geometry that,

- closes the gap
- represent other geometry well

and then extract new geometry from this mesh.

m5edr July 9, 2013 10:52

Quote:

Originally Posted by kad (Post 438701)
In ICEM it is very hard to fix. First you could go back to your CAD tool and try to fix it. Or try another exchange format.

this is easy for me , i'm using solidworks then i export the file as IGES , ACIS , Parasolid or STEP format (i used ACIS among of them) , then i send the file to AnsysGeometry to get rid of solid part in blade and hub.

Anyawy I will try other exchange format, thanks Kad

kad July 9, 2013 11:09

I think it is possible to export solidworks geometry directly from solidworks to Designmodeler and from there to ICEM via workbenchreader. Maybe you have to adjust your CAD configuration manager. Check this video:

http://www.youtube.com/watch?v=6yyPC9gXZZ8

Or you can only use the workbenchreader in ICEM for solidworks data. This should be somehow more "lossless" because you avoid converting back and forth.

m5edr July 29, 2013 00:11

Error appears again
 
Hi, All

I forced to change the mesh size specially on blade surface (for accurate mesh presentaion on Fluent and hence accurate results) , So Massage appears again "repair holes" if i press YES a internal screen massage of "faces are missorinted"

However i upload the new ICEM file (http://www.4shared.com/rar/0WbPTjkJ/Gometry.html) , I ask for a definitive solution for this problem

Thanks in advance

m5edr July 29, 2013 11:10

I forgot to say that i'm tired all the above ways to avoid the problem BUT the error still continue


All times are GMT -4. The time now is 17:42.